Drilling, Boring, and Hole-Making Toolpaths

Hole-Making Toolpaths in Mastercam

Hole-making is one of the most common operations in machined parts. Mastercam groups all hole-making operations under its Drill toolpath category, which calls on canned cycles that your CNC control executes in a single block of G-code. Understanding how to choose the right cycle, set the correct parameters, and sort holes efficiently is essential for productive, accurate work.

The Canned Cycle Toolbox

Each operation below maps to a standard G-code canned cycle supported by Haas and most FANUC-compatible controls.

Spot Drill (G81 or short G82 dwell): The first operation in almost every hole sequence. A spot drill creates a shallow conical indent that guides the following drill and prevents it from walking. Without a spot, a twist drill can drift and produce an off-location hole. Set depth just deep enough to chamfer the full drill diameter—typically one-half the spot drill's included angle depth. Never skip this step on critical bolt-circle or dowel-pin locations.

Drill (G81): A standard drill cycle feeds to depth, then rapids out. Use it for shallow holes (depth ≤ 3× drill diameter) where chip evacuation is not a concern.

Peck Drill (G83 – full retract): The drill feeds to a peck increment, retracts fully to the R-plane to clear chips, then re-enters with a small clearance before the next peck. Use G83 for deep holes (depth > 3× diameter) and gummy materials such as aluminum or stainless. Full retract ensures chip evacuation but adds cycle time.

Chip-Break (G73 – partial retract): The drill feeds to a peck increment, then retracts a small fixed amount (often 0.010–0.020 in) to break the chip without fully clearing the hole. Faster than G83 but relies on chip fragmentation; not appropriate when chip packing is a risk.

Tap (G84 – right-hand rigid tapping): The spindle feeds in at a synchronized feed rate (feed per rev = pitch), then reverses RPM and retracts. Rigid tapping requires a control that supports spindle-encoder feedback. Feed rate must exactly equal RPM × pitch; Mastercam calculates this automatically when you enter the tap's pitch and desired RPM.

Bore (G76 or G85): Used when hole size and finish must be held tightly. A boring bar feeds to depth at a precise diameter; G76 uses an oriented spindle stop for a clean retract without marking the wall.

Selecting Peck Increment

For deep-hole drilling, a starting rule is peck increment = 3× drill diameter, then adjust based on material and observed chip character. Smaller pecks help in hard or stringy materials; larger pecks reduce cycle time in free-machining steel or plastics. In Mastercam's Drill parameters page, enter this value in the Peck field. You must also choose between G83 (full retract) and G73 (chip-break) using the Cycle drop-down.

Point Sorting: Why It Matters

When a pattern has many holes, the order in which the machine visits them affects non-cutting (rapid) travel time. Mastercam offers several sort methods:

• Shortest path (2D optimization): The control visits holes in an order that minimizes total rapid distance—similar to a traveling-salesman solution. This typically yields the fastest cycle time for large random patterns.
• By-diameter grouping: All holes of one size are drilled before moving to the next size, reducing tool changes on multi-diameter patterns.
• Rotary sort, bounding-box sort, and others are available for specific part geometries.

Always run a Backplot after changing sort order to confirm the tool path looks correct and no collision with clamps or fixtures is possible.

Tap Drill Sizing

Before programming a tap cycle, you must drill the correct tap drill size. Use a tap drill size chart or Machinery's Handbook to find the recommended tap drill diameter for your thread specification (e.g., ¼-20 UNC, M6×1.0). Drilling undersized will break the tap; oversized reduces thread engagement below the minimum required for strength.

Setting Up the Tap Cycle in Mastercam

1. Select Drill toolpath and choose the tap tool from the library.

2. In the Cycle drop-down, choose Tap (maps to G84).

3. Enter pitch (e.g., 0.050 in for ¼-20; this is 1÷20).

4. Enter desired RPM (follow tap manufacturer recommendation; carbide spiral-flute taps can run faster than HSS hand taps).

5. Mastercam automatically computes feed rate = RPM × pitch. Verify this value before posting.

6. Set depth to full thread depth plus approximately 2–3 thread pitches for lead-in.

Safety in the Lab

Even though this lesson is simulation-based, establish safe habits now:

• Backplot and Verify every toolpath before posting G-code. Collisions identified in simulation cost nothing; collisions on the machine can injure operators and destroy tooling.
• When the resulting G-code is later run on a machine, apply lockout/tagout (LOTO) procedures before any setup or tool change, per OSHA standards.
• Wear safety glasses whenever you are near an operating machine.
• Never override a tap cycle mid-program on the machine without understanding spindle-reversal logic; an interrupted rigid tap cycle can break the tap in the hole.

Backplot and Verification

After building your toolpath sequence, run Backplot to animate tool motion and check point order, rapid moves, and cycle depth. Run Verify (solid simulation) to check for gouges. If Mastercam flags a warning—such as a peck depth that exceeds the hole depth—read the message carefully, identify the parameter in error, correct it, and re-verify before posting.